So still very green on most 3d modeling software but I am 3d printing a lithoplane and wanted to cnc a stand for it but need help getting the stl file into something I can use.
I’ve tried Freecad as that’s what I’ve been trying to learn but the complexity of the stl causes it to crash when I try to use it as a pocket feature
Most CAD software is not built for super complex 3D modeling.
What exactly are you trying to do? Are you just trying to model a stand for a specific lithophane? Your best bet might be to just model a sample of the lithophane to correct dimensions and model a stand around that.
Otherwise, you might need to do it something like Blender.
You can also import the STL into Blender and simplify it, or cut off the parts that are unnecessary for creating the stand, for example, if you only need the bottom 1/4 of it in the model in order to model the stand.
Oh I didn’t think of that. I use mesh mixer for some of the 3d print files I mess with. Maybe make that work
Yes used a website generator and went with a curved design as that’s what looked best. Just trying to simplify the process vs wasting material for what will be a one off project. The biggest reason I want the stand vs doing some 3d print model is I’m going to be adding text to the stand and want to make it look as nice as I can
Yep, then Blender or Meshmixer is probably your best bet is to chop off anything you don’t need in order to model the stand.
Just something to reduce the number of triangles so the CAD program can cope with it.
@Peacester are you able to share your .STL here or in a DM (I promise not to share if it is IP/sensitive ). If the 3D model is not too complex, then my FREE HoloZens app might be able to help with regular STL to SVG conversion (even if you don’t want to make holograms).
I can generate an example .SVG from your .STL to see if that’s the kind of thing you’re after.
EDIT: Sorry, I messed up, and misread what Andrew’s looking for. HoloZens can’t help for this. HoloZens would be a better fit for converting low/simpler .STL models with a flat front face(s) to .SVG. Andrew’s looking for a stand, completely different. Suggested Fusion 360 and OpenScad and some ideas in our DM…
I’ll send you it once I get back to the computer. Lithoplanes I feel are usually complex and that’s my issue with freecad but a dedicated software I feel like should be able to do it
Also how did I miss this hologram app you made. I try and be on here a bunch and have you subscribed! 
@Peacester showed me the neat FREE Image to Lithophane tool at https://3dp.rocks/lithophane, his topic inspired me to take a deeper look.
Originally planned to spend ~30mins making a quick design and 10min video… Ended up with this several hours later… 
Here’s a basic stand video and files that hopefully helps people new to Fusion 360 who are looking to do this type of project.
Goal was to provide a Fusion 360 intro for a common project scenario, sharing a few ways in which you can use Fusion 360 to carve out the profile of any 3D model from a flat piece of stock.
stand.zip (16.2 KB)
0:00 Intro — WHAT, WHY and HOW to use Fusion 360 to create .STL and .DXF files for a basic stand. We’ll design the stand with material cutout for matching the bottom profile of an existing .STL model to be slotted into top of the stand. The resulting .STL and .DXF files can be made real using a CNC, laser or 3D-printer to help support a Lithophane of Mercury (our Cat).
1:00 Use FREE opensource Image-to-Lithophane tool to generate .STL models with embossed shapes.
3:20 Generate a high resolution and low resolution Lithophane models. We’ll use low res model to help Fusion carve out a profile in the stand.
5:25 Fusion 360, insert .STL file as a mesh, then convert to Solid Body. Solid Body objects are easier to modify than meshes.
6:40 Examine model being supported, figure out plan for Stand sketch and model.
7:50 Slice/Split Lithophane model, so easier to focus on creating profile being recessed into Stand.
9:00 Sketching profiles by manually eyeball tracing a geometry shape using lines, 3 point Arcs, etc…
10:10 Sketching profiles by Projecting specific geometry features (surfaces, edges, points) using lines, 3 point Arcs, etc…
12:40 Plan to sketch profiles by Projecting entire Solid Body’s geometry features onto Sketch plane.
14:40 Plan to split/slice Cat Lithophane body into 2 parts. Will hide embossed area, just work with section that will recess into stand.
16:00 Creating Offset Construction plane to use as tool for splitting.
16:50 Note on triangles/surfaces were simplified by split operation. Helps Fusion 360 performance/responsiveness.
17:30 Actually sketch profiles by Projecting entire Solid Body’s geometry features onto Sketch plane.
18:35 Start sketching Stand outline.
19:10 Using Dimension Constraints to setup size/layout. Mindfully create so design works even if some dimensions are changed (e.g. Length and Width).
20:40 Virtual construction lines for helping align/center objects.
22:00 Creating Symmetrical constraint to center cutout profile within stand.
23:30 Short note on over constrained models.
26:20 Vertically center cutout profile within stand by using dimension constraints that reference other dimensions, and using basic math/equations.
27:00 Short aside… Clarifying terms, what are Constrained versus Driven Dimensions.
29:00 Vertically center cutout profile continued…
30:30 Sketching rounded corners.
31:15 Fixing symmetry dimension constraint broken by adding rounded corners.
33:00 Make the model “Parametric”, so easier to edit, by adding parameters that change Length and Width dimensions using Solid » Modify » Change Parameters.
34:45 Adding Offset profiles for gap tolerance.
36:00 Exporting Fusion 360 Sketch to .DXF.
36:20 Creating 3D model by Extruding Sketch profiles.
38:30 Use Offset extrude to help raise Stand body, so the Lithophane is recessed/embedded (with contour gap).
39:30 Extruding more material that joins existing to help fill void/hole.
42:42 Changing material and color appearance.
44:00 Exporting models as .STL. Can export entire group, or individual models.
Guy ask for some input and you make a 36 minute video showing him step by step how to do it. Can somebody give @azab2c an award!??
Seriously. Above and beyond! Taught me some good things about CAD too
Most welcome. Just shared how I’d do this, late at night… Am no CAD pro, so am hoping others here will call out bad/misleading advice I shared. Hopefully more experienced folks here, and there are many, will help share more efficient CAD methods/considerations to help elevate all of us.
Or maybe, non CAD approaches too… e.g fwiw the interesting image-to-lithophane project is open source, so, someone could fork and mod the project (looks angular and three.js based to me) to just auto generate downloadable .SVG representing the footprint profile for the current lithophane.
Off camera, I tried out a few other things like using Merge to cut the lithophane body out of the stand, potentially without needing to create a sketch even.
For this project, that’d be a faster/simpler approach than what I showed. But trying to use Push Pull operation to add 0.5mm gap tolerance ended up with unwanted artificats/behavior…
For this project, could avoid using Fusion’s push/pull and it’s quirks for this profile, and, instead use EstlCam’s features to achieve desired gap tolerance.
Cheers!
